This is something I have been wondering about for a while, and reading the thread about building the TubelabSE as a P2P amp stirred it up again:
Ok...if two wires side by side (co-planer) create inductance and/or stray capacitance, how is this issue addressed in PCB design? It seems to me that PCB would be a breeding ground for this??? PCB is the co-planer poster child it would seem. Please keep in mind that I am a noob and that my expeience is pretty much confined to P2P and tag boards with flyoffs.

It's generally not a problem at low-ish frequencies like audio. With high speed circuits, it can be a problem. Sometimes guard traces are run between traces where coupling would be an issue. But for sub-megahertz stuff, trace to trace coupling is pretty small. Remember, in the old days, lots of wires were bundled together in harnesses...

Ok...if two wires side by side (co-planer) create inductance and/or stray capacitance, how is this issue addressed in PCB design?

Quote:

It's generally not a problem at low-ish frequencies like audio.

Two traces side by side can and do create coupling between them. It is usually a problem in high speed digital circuits, and RF circuits. It can be a real problem where both must coexist. Throw in some low level audio and shrink the whole thing down to a couple of inches, and you have the worst possible PC board environment. We call them cell phones, and I spent several years of my life learning how to lay out those PC boards. The worst ones are the ones that pulse the transmitter on and off tens or hundreds of times a second (iDEN and GSM). It is real easy to let the pulsing RF corrupt the audio or whack the frequency synthesizer. We fix this with guard traces, multiple layer boards with multiple ground planes. All of the high power RF and high speed digital stuff is confined to a few layers sandwiched between ground planes, and the audio is several layers away, again sandwiched by ground. We use multi kilobuck PC board layout and simulation tools from Mentor Graphics and Cadence to assist us in getting this stuff right. It still requires some itterative design cycles.

This sounds like the way to design a tube amp, right? NOT! Why? The circuitry in a cell phone is all low impedance, and the audio is purposely not HiFi. A few hundred pF of stray capacitance to ground is a good thing in a phone, it rolls off the highs, and keeps the RF out of the microphone, earpiece, and speaker circuits.

Vacuum tube audio equipment is all very high impedance stuff. The input impedance of a vacuum tube stage can easilly be 1 megohm. A few hundred pF to ground will make it sound like a cheap AM radio. A few pF of coupling to another circuit can make an oscillator. I have spent a few years figuring out that laying out a PC board for a vacuum tube audio amp requires a similar skill set, but some very different rules. These rules are not unlike a PTP design. You do not want to run a high impedance line like a grid circuit, with ground on the opposite side of the board. You must be very careful about the power supply currents (as in PTP) to avoid hum. When signal lines must cross other lines they should be at right angles. Multiple ground planes are not needed, or wanted. There are zillions of little details, and like the RF world where I work full time, I discover new ones with every board.

If you have the knowledge and ability to do PTP right, you can build a very good amp. I have built several. Get it wrong and you may have an amp that hums or oscillates. Often the amp can be fixed without a total rebuild, but some (often frustrating) tinkering may be needed.

If a PC board layout is not right it can also oscillate or hum, or the frequency response may be rolled off. Often the only remedy is to salvage the expensive parts, and toss the rest. Then you can lay out another one, make the PC board, populate it (put all of the parts in) and try again. Some boards work with minimum fuss, and others take several tries to get right. I did 6 or 7 versions of the Tubelab SE before I was happy with it, but the Simple SE only took two.

All of this is a lot of work, and the amount of work goes up very quickly with the complexity of the circuitry, and the component density. Yes it is a lot of work, but the real advantage of using a PC board, is that once it is done right, they will all be EXACTLY THE SAME! The amp can be assembled by an inexperienced builder since all of the hum and oscillation demons have been designed out already if the board was designed properly.

__________________
Tubelab, it's 5 year mission. To explore strange new tubes, to seek out new circuits and topologies, to boldly go where no tube has gone before......

Originally posted by tubelab.com Two traces side by side can and do create coupling between them. It is usually a problem in high speed digital circuits, and RF circuits. It can be a real problem where both must coexist. Throw in some low level audio and shrink the whole thing down to a couple of inches, and you have the worst possible PC board environment. We call them cell phones, and I spent several years of my life learning how to lay out those PC boards.

Being an EE but coming from the software side...I dunno how you guys design these things. They're insane.

I design small multi media recorders and while not quite as small as a cell phone - great care must be taken when you have audio, video and high speed digital busses, DSP's (plus switching power supplies) all in a very confined space. Ground planes, trace separation and impedance matching are your friend in these designs.

One of the most interesting things is that the components are so small - resistors and caps - that we do a lot of our work under a microscope. And, I have to be extremely careful not to drink too much coffee that morning, or it makes rework even more of a challenge...

I am curious why a good ground plane doesn't help with noise isolation. I can understand that impedances need to be high, but you can do that with changing the geometry of trace width to plane... are they really so high that an .062 pcb can't accomplish this?

Leave PC boards to the cell phone and computer gurus. Build your audio preamp and amp with point to point. There is just too much "black art" to PC board design. You can wind up making a swell capacitor easily. And replacing tubes puts too much torque on PC pads. Ray Hughes

__________________
" Polarities are seldom aware of their polarness." Prospero

Originally posted by bereanbill This is something I have been wondering about for a while, and reading the thread about building the TubelabSE as a P2P amp stirred it up again:
Ok...if two wires side by side (co-planer) create inductance and/or stray capacitance, how is this issue addressed in PCB design? It seems to me that PCB would be a breeding ground for this??? PCB is the co-planer poster child it would seem. Please keep in mind that I am a noob and that my expeience is pretty much confined to P2P and tag boards with flyoffs.

It tends to be a problem with high impedance tracks.
You can get crosstalk.

You could go for a hybrid design with the heaters run by wires and the rest on a PCB.

Take your Grandpa's statement to heart! Leave PC boards to the cell phone and computer gurus. Build your audio preamp and amp with point to point.

Well, I have designed cell phones, computer boards, countless other electronic gizmos, AND audio amplifiers (both tube and solid state) and I AM a Grandpa!

Quote:

There is just too much "black art" to PC board design.

There used to be. Now there are simulators and field solvers that take the magic out of PC board design. These tools are far beyond the financial reach of all but the big corporations. That is one of the few advantages of working in such a place. Using these tools on complex designs affords the experience needed to be able to do simple audio amps without them.

As is the case with PTP the most complex task of any PC board design is component placement. I will usually spend more time aranging all of the components on the PC board than the rest of the layout. It is not unlike a chess game where you must be able to visualize all of the routing needed to hook up a component and be able to think ahead to see how it will interact with the rest of the components. I have spent several days placing the components on a multi layer RF board, and then completely routed it in a few hours. Some people (my boss included) never get this important point.

Quote:

You can wind up making a swell capacitor easily.

Yes, this is the case with PTP too. if you think about it there is capacitance between ANY TWO conductors in an amplifier, be it PTP or PCB. The trick is to minimize the important ones. A good amplifier (or any analog circuit) designer understands this and works within his construction medium to achieve the desired result.

I have proven with the Tubelab SE and the Simple SE that it is possible to build an amplifier using PC boards that is just as good as a similar amplifier made properly with PTP construction. I have built several other vacuum tube amplifier designs over the past 40 years, and until about 10 years ago they were ALL PTP. I will admit that some of my first PCB designs didn't work too well, but that is how you learn. I will do a PCB for a tube amp now if there is ANY possibility that I am ever going to build more than one. Do I still use PTP? Yes, every design that I do starts off with some sort of PTP prototype. I haven't built a complete amplifier using PTP wiring in several years though.

PC boards are just another tool in the amplifier designers tool box. It it however a tool that requires knowledge and experience to use correctly, and like many hard to master tools, it can be feared or shunned by those who haven't mastered its use. As with any complex tool, there must be some reason to justify overcomming the barriers to its use. The big reason for using PC boards is repeatability. Once a PC board is PROPERLY designed by a competent designer, they will ALL be identical. This PC board can then be used by an inexperienced builder to make an amplifier that works exactly the same as the original. This is not the case for PTP construction unless a very detailed set of plans are followed exactly.

Quote:

And replacing tubes puts too much torque on PC pads.

This is another one of the reasons that I hear for not using PC boards. There are several, most of which were true at one time, but don't apply today. I worked in a TV repair shop in 1969 - 1970. PC boards had been used in AA5 radios since the late 50's and in TV's since the early 60's. They used to be made of a phenolic material that positively sucked! The traces would come off if you touched tham with a soldering iron, and yes, yanking the tubes too often broke the traces right at the socket. The boards themselves were microphonic and absorbed moisture. This was a real problem in south Florida in a time when only well to do people had air conditioning.

This type of PC board was often used in HiFi equipment with equally bad results (early Dynaco comes to mind). These "truths" are still propagated today, even though they are no longer true. A modern PC board with oversize pads for all of the parts (one of my "secrets") is very hard to destroy, and I have run so many tubes through some of mine that I have worn out the sockets, replaced them, and worn them out again. In fact there is a Simple SE board sitting on my workbench that has been used for most of my glowing tube experiments for over two years. Every component in that board has been changed several times, and the PC board itself is still in good shape.

I am curious why a good ground plane doesn't help with noise isolation. I can understand that impedances need to be high, but you can do that with changing the geometry of trace width to plane... are they really so high that an .062 pcb can't accomplish this?

Yes. The grid circuit impedance of a vacuum tube is inherently very high. Because of this a few pF of capacitance to ground could cause high frequency roll off. The standard practice of running a trace over a ground plane will cause problems. In order to solve the reliability issues associated with PC boards and replacing tubes or components, I like to use a minimum trace width of 50 mils and a minimum pad size of 100 mils, often larger. A 50 mil trace over ground on a .062 PC board has a characteristic impedance of about 50 ohms depending on the dielectric constant of the board material. Even a short 50 ohm runner will be very lossy in a 100K ohm circuit. So the trick here is to isolate these traces, and remove the ground plane from underneath them.

Quote:

You could go for a hybrid design with the heaters run by wires and the rest on a PCB.

High current AC heaters can be a problem on a PC board. There are two ways to solve this. In the Tubelab SE, I use DC heating for all heaters. No AC, no hum. In other amps the heater traces are routed as a differential pair. I have found that in some cases they want to be run over a ground plane, and in other cases they want to be isolated. How do I know which works best? I run the traces over a ground plane in the first pass board. After the amp is working, I make hum measurements, then remove the ground plane with a Dremel tool, and test again. It isn't easy, but I have done similar stuff with a phone board too.

__________________
Tubelab, it's 5 year mission. To explore strange new tubes, to seek out new circuits and topologies, to boldly go where no tube has gone before......

Most of us are amateurs not manufacturers and we are are only building one or two pieces and we would like them to work the first time. I agree with Tubelab's assumptions but if I were an amateur just building for the first time I would not advise them to buy a PC board layout software program and attempt a circuit board design. Ray Hughes

__________________
" Polarities are seldom aware of their polarness." Prospero